Post-processors

A post-processor is a small TOML file (name.toml) and a Jinja template (name.*.j2); see Post-processors for writing your own. The TOML file’s fields:

The file

Field	Type	Required	Meaning
`arcs`	boolean	no	Write arcs as G2/G3; false writes them as short lines (G1). Missing: false.
`decimals`	integer	no	Decimals for coordinates and feeds in mm. Missing: 3.
`file_extension`	string	no	The G-code file’s extension, e.g. `.nc`. Missing: `.nc`.
`inch_decimals`	integer	no	Decimals for coordinates and feeds in inches. Missing: 4.
`name`	string	yes	The post’s display name, e.g. “GRBL”.
`note`	string or null	no	A word for the operator, shown on the setup sheet, e.g. that the post isn’t tested on a real controller yet. Missing: none.
`schema_version`	integer	yes	The version of the settings format: 1.
`spindle_dwell_s`	number	yes	Seconds to wait after starting the spindle, for it to reach speed; 0 for none. Required: a silent default could start cutting at low speed.
`template`	string	yes	The template’s file name, next to this file, e.g. `myrouter.nc.j2`.
`tool_changes`	list of ToolChange	no	How the template can write a job with several tools: `files` (one program per tool), and `program` (one file with tool changes) if the template writes them. Missing: files only.
`units`	list of Units	no	The units the template can write: `mm` (G21) and `inch` (G20) if it writes `{{ units_word }}` instead of a fixed G21. Missing: mm only, so a machine set to inch is refused rather than given inch numbers under G21.
`written_by`	string or null	no	Who or what wrote the file, for reference.

ToolChange

How a job with several tools is written.

"files": One G-code file per tool group; the user changes the tool and sets Z zero between.
"program": One file with T<n> M6 at each change, for a sender that handles it.

Units

One of: "mm", "inch".

Built-in post-processors

Name	File extension	Decimals	Arcs	Spindle wait (s)	Tool changes	Note
`grbl`	`.nc`	3	G2/G3	3	files, program
`linuxcnc`	`.ngc`	3	G2/G3	3	files	Not yet tested on a real LinuxCNC machine: check the program and air-cut first.
`mach3`	`.tap`	3	G2/G3	3	files	Not yet tested on a real Mach3 or Mach4 machine: check the program and air-cut first.